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Problems with complex sweep and guide faces.

6 REPLIES 6
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Message 1 of 7
kevinventor
633 Views, 6 Replies

Problems with complex sweep and guide faces.

Hi all, first poster here.

 

I am having problems with a complex sweep. I wish to produce two elliptical grooves in a radial face. The groove centreline is perpendicular to the radial face. The sides of the groove are parallel to the groove centreline. The groove depth is 3mm, parallel to the radial face.

Unfortunately the grooves do not follow the same path so I cannot model them together.

 

I can model either one of the grooves individually, but once I have modeled one, I can not model the second groove, which ever order I model them in. (I have tried suppressing the first groove before modeling the second, which works until I unsuppressed it again.)

I think the problem lies with the guide surface selection. When cutting the first groove I can select the entire radial face as a guide surface. But once the first groove is modeled, I obviously can no longer select the full radial face as the guide surface. It will let me select the face either side of the first groove, and will even show me a preview that looks fine. But once I hit OK I get the "Modeling Failure in ASM. Redefine Inputs) message.

 

I have attached an image to try and help my explanation, unfortunately I will not be able to upload the model.

 

Thanks in advance.

Kev.

 

Groove 1.JPG

 

 

 

Groove 3.JPG

 

 

 

Groove 4.JPG

 

Groove 5.JPG

 

Groove 6.JPG

 

 

 

 

 

 

 

 

 

Groove 7.JPG

 

 

6 REPLIES 6
Message 2 of 7
JDMather
in reply to: kevinventor

From the state of the image you attached -

Save As a copy

right click on the End of Part marker and select Delete all features below EOP.

Drag the red EOP above all remaining features hiding them.

Save this copy file with the EOP in a rolled up state.

Right click on the filename and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here.

 

If you still can't upload the model because of proprietary information, surely you can create a dummy part that exhibits all the behavior of your actual part (doesn't look like much there in the area of interest) and attach it here.

 

The Sweep tools might allow you to get your design intent without surface modeling.

If not, some variation of this might help http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%2011.pdf

 and

http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%207.pdf


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Message 3 of 7
glenn-chun
in reply to: kevinventor

Hi Kev,

 

It is difficult to reproduce the issue without having the model.  Since you cannot upload the model here, please send me the IPT file by email.  My email address is glenn dot chun at autodesk dot com (Replace dot and at with . and @, respectively, and delete spaces.)

 

Once I receive your model, I will find out whether this is a user error or defect and try to suggest a solution or workaround.

 

Glenn

ASM Development



Glenn Chun
Sr. Principal Engineer
Message 4 of 7
kevinventor
in reply to: glenn-chun

Please find the attached zip file containg the model in question.

Message 5 of 7
kevinventor
in reply to: kevinventor

is there an issue with adding attachments to posts at the moment, or am i doing something wrong?

Message 6 of 7
glenn-chun
in reply to: kevinventor

Hi Kev,

 

I reproduced the issue that you're experiencing.  Your guess was indeed correct -- It is an Inventor defect against collecting guide faces.  Let me explain the problem and show you a workaround.

 

Since we want the green face to be the only Guide Surface, we click on the green face.  Inventor preview shows correctly because Inventor passes the green surface to ASM (Autodesk ShapeManager, the geometric modeling kernel for Inventor).  Once you hit OK on the Sweep dialog, Inventor somehow collects both green and red faces and send them to ASM.  Sweep fails in ASM because the given guide faces are disjoint.  I logged defect 1502140 against this issue.

 

1.png

 

The following is a workaround that I came up with.  Create an Offset Surface using zero distance.

 

2.png

 

For the Guide Surface in sweep, select the face of the Offset Surface feature, not the green face.  If you hover your mouse over the overlapping faces for a few seconds, you will see the Select Other tool.  The second face should be the one from the Offset Surface.

 

3.png

 

In Inventor 2011 or earlier, you will see the following glyph after mouse hovering.  Click the right arrow to select the second face and then click the green dot in the middle.

 

3a.png

 

Sweep should create the second groove successfully because Inventor passes only one face to ASM this time.

 

4.png

 

Finally, turn off the visibility of the Offset Surface:

 

5.png

 

Hope that helps,

 

Glenn

ASM Development

 



Glenn Chun
Sr. Principal Engineer
Message 7 of 7
kevinventor
in reply to: kevinventor

HI Glenn.

 

I followed the work around you sent me and it has worked.

Thanks for the help!

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